NX 7.5 Part Configurations

[mike734]

Hello all. I used to be able to make different part configurations in SW which would suppress or unsuppress certain features in a part.

I have a part that will have tapped holes at the assembly level, but not as a component. In the past I would have two configurations of this part in the same part file i.e. "w/ holes" which has the hole features unsuppressed and "w/o holes" which has the holes suppressed. In assembly drawing it would show the "w/holes" in a particular view and may show the "w/o holes" in another view. These would be 2 different assembly "configurations".

How is this possible in NX? I would like there to be an arrangements function to be used with features for part files in addition to parts for assemblies. Since I can't add the holes at the assembly level without making the part a linked body (don't like to do this), how can this be accomplished?

Thank you,
Mike

 

[PrintScaffold]

You can add the holes at the assembly level without making the part a linked body.
What you need is promotion. Insert > Associative copy > Promote body.
Try it. It's not the same as creating a linked body.

 

[JohnRBaker]

While the 'Promote' body approach described by PrintScaffold is the one which duplicates the actual 'manufacturing' workflow the best and therefore would generally be considered the recommended approach to follow, there is another option that you might want to look at. That is create your Threaded Holes in the peice part and then use Suppress-by-Expression to control whether they are there or not. Then from the assembly where the part is used, you can use Interpart Expressions to override the value of the Expression controlling the suppression of the threaded holes. Now if there's going to an on-going need to use this component, sometimes with the threaded holes and sometimes without, you can go one step further and take the piece part, complete with the Threaded holes and the expression to control their suppression status and create a 'Part Family' where one version will have the threaded holes and another one would not (becasue the suppression expression was been set differently in that version of the component). Then when you add this component to an Assembly you'll be given the option to use the one with the threaded holes or the one without. I suspect that this last option, using Part Families, will get you the closet to what the SolidWorks 'Configuration' scheme provided you.

John R. Baker, P.E.
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To an Engineer, the glass is twice as big as it needs to be.

 

[PrintScaffold]

A valid point, John.

I only gave a hint than modification of a part geometry in the assembly context can be made without creating a WAVE-link.